Programming a HMC w/ Rotary Table (B axis)

[Kampfzentrum]

Could really use some help here, I am programming for a Toshiba HMC with rotary table. I'm able to create the various axis I need to get the toolpaths right, but I cannot get the table to move. Shouldn't it move automatically? Is that information in the post? Or am I missing something?

I have seen previous posts talking about how this all works, if someone knows, please direct me. Otherwise, I could really use some help.

Thanks.

[neurosis]

More information might help. 

Is it not outputting any rotary movements at all?  Are the rotary moves in the program but the table is not moving?

Do you have a sample file that someone could look at?

[?Mark]

Did you add a rotary to your machine definition and is the post supporting it at all?

[Kampfzentrum]

I'm really sorry if I was vague. Basically, yes, the table is not moving. Despite that I create various axis, the table always is set to B90. even when it moves to a tool that I have programmed to another plane. I used numbers 0, 1, 2, and 3 to denote each movement (say each 90 degrees)I'm really sorry if I was vague. Basically, yes, the table is not moving. Despite that I create various axis, the table always is set to B90. even when it moves to a tool that I have programmed to another plane. I used numbers 0, 1, 2, and 3 to denote each movement (say each 90 degrees).

Mark, I did not create the machine definition and I am in talks with ShopWare now to figure out if the post supports it. I am hoping so. I'm just wondering if I am doing something wrong. I'm going to create a BS program now to show you guys.

Thanks for the attention.

[Chris In-House Solutions]

Hey Kampfzentrum,

To change your table you should just need to change your tool/construction plane.  Front is typically B0, Right/Left would be B90 or B270 (-90) and back would be B180.  WCS should be setup to TOP.

[Colin Gilchrist]

To program a Horizontal Machine in Mastercam, you must use TOP WCS, and FRONT T/C Plane, for B0.

Using the "Standard Planes" in Mastercam, (all OPS use TOP WCS), this is what you should get:

Front = B0 = G54

Right = B90 = G55

Back = B180 = G56

Left = B270 = G57

The Work Offsets are set to be "created automatically", each time that a new Tool Plane Rotation, is detected inside the Post. The issue, is that if you were to "insert" an Operation, that didn't use one of the "standard" (90 degree) planes, it would use "the next available work offset number".

To avoid that happening, inside the Planes Manager, you should explicitly set a Work Offset Number for each Plane that you use. Every Plane must be a "rotation of the Front Plane", about the Y+ Axis of the Front Plane. Only the XZ vector directions should change. Otherwise the Post will give you an error.

What this means is that you likely need to reprogram your part, since you programmed it from "Top"...

[neurosis]

1 hour ago, Kampfzentrum said:

Mark, I did not create the machine definition and I am in talks with ShopWare now to figure out if the post supports it. I am hoping so. I'm just wondering if I am doing something wrong. I'm going to create a BS program now to show you guys.

 

If you think that youhave your planes set right you can use one of the generic hmc machine def and posts that come with mastercam to test.

 

Do those install by default now?     I cant remember.

 

Otherwise post a file for someone to look at and it should be pretty easy to figure out.

 

 

[Colin Gilchrist]

Your other choice is to use a "VMC" type Machine Definition, Control Definition, and Post, and to configure the "Rotary Axis" to rotate about Y+ of the World WCS. You should also set the Starting 0 Degree position to "Z+".

[Clarence L Cook]

If the B axis information is in the nc file and still not rotating, I would look to codes to unlock and lock the rotary axis.  On my Makino, they are M11 and M10.

[TFesta]

Colin , How do I turn off the work offset changing part? I want to keep the same work offset, I don't need it changing every index.

Thanks.....Tim

[jlw™]

Unless you use the switch in the post to always output a certain offset you need to define it in the plane manager:

[Colin Gilchrist]

19 hours ago, TFesta said:

Colin , How do I turn off the work offset changing part? I want to keep the same work offset, I don't need it changing every index.

Thanks.....Tim

Like Jeremy mentioned, assign "0" to each "Plane" being used in the Planes Manager. This will output 'G54'. 1=G55, 2=G56, ect.

So if you want "G57" for all output, assign '3' to each Plane.

[TFesta]

I have MC X6. I did what you said and it made the indexes G54 But then made the Front G55. I use to program all the time with the rotary table (MC X5) but it was not a work offset machine so no problem.  Where in the post do I turn it off at? I was thinking of just changing the G54, G55, ect to all G54's. Not the best way but it's a fool proof way. The MC X6 post is a little bit different then MC X5 and I can't find the switch.

[jlw™]

Can you share a file?

[TFesta]

I'll have to get the program from work, I work swing and I'm home right now. This job doesn't have internet on the computer that I use or I would have been done and solved weeks ago. It won't be much of a post. Each time I index it changes the work offset. I'll try and change the default setting and see if that will fix it. But it looks like I have to set it at every plane change.

[TFesta]

Ok. I can set it like you have listed. Thanks for your help. Have a great weekend.

[shimoorthy]

On 2/10/2018 at 2:48 AM, TFesta said:

Colin , How do I turn off the work offset changing part? I want to keep the same work offset, I don't need it changing every index.

Thanks.....Tim

use plane tap in parameter menu and click work offset manual and enter 0 ,1,2,3 . 0=G54,1=G55,2=G56,2=G57

Its reflects in same as any plane set every view in same value.